Wondering if this swept profile is possible

[Siress]

This is the type of check valve found in veins. I would like to know of a way to model these valves quickly. My intuition was that I could revolve sweep the profile with a constraint on the inner diameter of the tube. This doesn't appear to work (although it showed a preview of such while I was playing around with the settings...go figure.)

Any help would be appreciated!
Thanks,
-Siress

 

[CorBlimeyLimey]

I can't quite fathom the shape you are trying to create from your model views.

From the inset image it looks like a simple revolve of the valve section would suffice.

 

[SBaugh]

I would venture to say probably not. For one the profile does not intersect the path. I would probably put the path on the other end where it would intersect the profile.

THe profile looks like its just 2 sketches and not a closed boundary. If its not closed then I would suggest that use a Surface sweep.

Its hard to say without having something more to work with.

Scott Baugh, CSWP

http://www.scottjbaugh.com

"If it's not broke, Don't fix it!"

faq731-376

 

[MadDogMcDurmott]

If I looked at that correctly, I would Loft with guide curves and Shell for wall thickness.

 

[TheTick]

For your sections, try using a partial ellipse or parabola instead of a spline. Splines don't respond well to guide curves in sweeps.

 

[Siress]

This is what I'm making, essentially:

http://www.gatech.edu/newsroom/release.html?nid=46488&source=1

I work with the group that did that project, but the way they did it requires a lot of operations. I was hoping to make it quickly, since the project I'm working on requires several of them. Compared to them, I've already made it a lot faster, but I would like to have it done in one operation like I mentioned in the first post. I'll try the suggestions later, and see if I can make heads or tails of it.

Thanks!

 

[TheTick]

Each of your guide curves (yellow) should be a separate sketch. You can do this quickly by using your yellow sketch as a master and using "Convert Entities" to bring each loop into its own sketch.

Don't forget to use a pierce constraint to attach your profile to the guide curves.

 

[ctopher]

Try the deform tool.

Chris
SolidWorks 09 SP4.1
ctopher's home
SolidWorks Legion

 

[Siress]

Sorry guys, none of the recommendations have solved this in one step; at least not by my hand. I rarely use some of these features, so it's likely that I'm missing something.

The problem I'm facing with the deform tool, which is completely new to me, is that these primary features intersect. Based on the tutorial and help files, I don't believe the tool can be used on single bodies.

 

[ChrisDuncan]

You can do what you're thinking but you can only have one path and the profile is going to remain a constant cross section throughout that path.

with this shape the closing part of the valve is going to have to be an offset of the larger outer oval, but the smaller oval is only used to extrapolate the location of the profile.

splines are better for the profile when you want a surface that has no joint lines.

 

[mjcole]

Challenge


Can you make it so that the bottom slot shape can be raised and have the now Horizontal Line rotate for closed condition?
This could be done a number of ways but my thoughts are 3Dsketch if not already done that way or Ruled Surface with an angle.

Michael

 

[ChrisDuncan]

Okay, here's the way to do it exactly like your photo.

using splines for the profile and the path.

first tried it like you did using the large upper path and got this (fail)

http://farm3.static.flickr.com/2545/4159916711_f1f6a8e0e4_o.jpg

then by picking the smaller path it worked, apparently it will build starting with the smaller path and going larger, sort of makes sense.

this is one spline sketch (smallest oval) for the path that is offset for all the other oval sketches

http://farm3.static.flickr.com/2712/4159889453_efbc52d9d0_o.jpg

http://farm3.static.flickr.com/2699/4160643932_2292e1922a_o.jpg

 

[Siress]

Those last two images aren't showing up: Photo Unavailable -flickr

Anyway, I didn't have a problem getting the preview in my picture to model. Sorry I wasn't clear on that. The problem with doing that is, when the outer portion is trimmed off, the geometry isn't want it needs to be on the inside wall; not to my liking, anyway.

I just find it hard to believe that this awesome program cannot solve the geometry the way I want, and much more believable that it's my deficiency in knowing how to provide the proper input. A dynamic profile is featured in several solidworks tools, so I'm sure it's capable.

 

[ChrisDuncan]

not sure what you're asking for, "outer portion trimmed off"?

you can get a profile to change shape as it sweeps with guide curves

here's one of the photos again that didn't show up, this is the successful loft with all splines.

 

[Siress]

Can you get a guide curve to make the outer shape to be circular, while the driving path is still the oval?

 

[ChrisDuncan]

That's a tough challenge, don't think it's happening with one operation, you can do it but the surfaces are warped. It's tough to even get nice surfaces with multiple operations.

 

[mjcole]

The Path typically works best as a simple shape the circle would probably be the best. The guide curves can then control the shape of the feature.

The Deform Tool does work on single bodies I believe. It requires that you pick a solid body then perform the operation. If you have two SolidBodies which you could create as unattached Extrusions or Thicken Features you can do a loft and get Tangency and Curvature Constraints for start and end of the feature.

I have a model that I can upload later. Another Feature to look at is the Boundary Solid which is in the Extruded Solid Flyout. It's like a boundary surface except you can create a Solid by picking boundaries in multiple directions.
For now I'll attach images of the Loft and Sweep approaches I used.

http://files.engineering.com/getfil...fb37d39&file=Valve-Challenge_SweepFeat_p1.PNG

http://files.engineering.com/getfil...76383c72&file=Valve-Challenge_LoftFeat_p1.PNG

http://files.engineering.com/getfil...3c8ecf6c&file=Valve-Challenge_LoftFeat_p2.PNG

Michael

 

[Siress]

That looks awesome, Michael! I'll study them later; finals week is here. If you could upload the model at some point, that would be much appreciated.

Thanks again!
-Siress

 

[mjcole]

Here's the model it's not finessed as much as I like so be forwarned. I created several configurations 00 is what I use as Default config name to make it show at top of list the Sweep config has the Swept version of the Feature and Loft has the lofted version.

File is 2009 format V E R S I O N code = 4100


Michael

 

[ChrisDuncan]

some very interesting methods there Michael

here it is with two boundary surfaces, (stitched and solid)
thanks to your tip of the adjacent (deleted) bodies to get tangencies

http://i941.photobucket.com/albums/ad252/cadcim/VALVE-1.jpg

http://i941.photobucket.com/albums/ad252/cadcim/VALVE-2.jpg